G50 and G51 CNC Code | Scaling | Milling

English CNC Wiki
1

G50 and G51 CNC Codes: A Comprehensive Guide to Scaling in Machining Centers

Introduction:

CNC machining often requires flexibility in adapting programs to different sizes or variations of a part. The G50 and G51 G-codes provide this flexibility through scaling. G51 activates scaling, allowing you to enlarge or reduce the programmed toolpath by a specified factor. G50 cancels scaling, returning the machine to its normal, unscaled state. This guide provides a detailed explanation of G50 and G51 as used in CNC machining centers (milling machines), covering their function, syntax, applications, differences between control systems (Fanuc, Siemens, Haas, Mazatrol, Mitsubishi, Heidenhain, and others), best practices, troubleshooting, and programming examples. This article is written for all levels of CNC users.

1. What are G50 and G51 (in Machining Centers)?

In the context of machining centers, G51 and G50 are G-code commands used for scaling the programmed toolpath.

  • G51 (Scaling ON): Activates the scaling function. You specify a scaling factor for each axis (X, Y, Z, and potentially rotary axes). Subsequent movements will be multiplied by these scaling factors.
  • G50 (Scaling OFF): Cancels any active scaling, returning the machine to its normal, unscaled state (a scaling factor of 1.0).

Key Concepts:

  • Scaling Factor: A numerical value that determines the amount of enlargement or reduction.
    • Scaling Factor > 1.0: Enlarges the toolpath. For example, a factor of 2.0 doubles the size.
    • Scaling Factor < 1.0: Reduces the toolpath. For example, a factor of 0.5 halves the size.
    • Scaling Factor = 1.0: No scaling (the default state).
  • Scaling Center: The point about which the scaling is performed. This is often the workpiece zero point, but it can be specified differently.
  • Uniform Scaling: The same scaling factor is applied to all axes.
  • Non-Uniform (Asymmetric) Scaling: Different scaling factors are applied to different axes (e.g., scaling only in X and Y, but not Z).
  • Mirroring: Negative scale factor can be used for creating mirror image.

2. Why Use Scaling (G51)?

Scaling offers several advantages in CNC programming:

  • Prototyping: Quickly create different-sized versions of a part to test fit and function.
  • Part Families: Machine parts that are geometrically similar but have different dimensions without having to reprogram the entire toolpath.
  • Shrinkage Compensation: Account for material shrinkage during processes like casting or molding.
  • Engraving: Easily resize text or logos.
  • Unit Conversion: Convert a program written in inches to millimeters (or vice versa) by using a scaling factor of 25.4 (or 1/25.4).
  • Simplifying Programming: In some cases, scaling can simplify the programming of complex shapes.
  • Creating multiple size variants

3. G51 and G50 Syntax and Parameters

The general syntax for G51 (scaling on) is:

G51 X[Scaling Center X] Y[Scaling Center Y] Z[Scaling Center Z] P[Scaling Factor]

Or

G51 X[Scaling Factor X] Y[Scaling Factor Y] Z[Scaling Factor Z]

And Some Controls:

G51 I[Scaling Factor X] J[Scaling Factor Y] K[Scaling Factor Z]
  • G51: Activates scaling.
  • X, Y, Z: These specify the scaling center (the point about which scaling is performed). If omitted, the current position is often used as the scaling center. This is a crucial point – an incorrect scaling center will distort the part.
  • P[Scaling Factor]: Specifies a uniform scaling factor (applies to all axes). For example, P2.0 doubles the size, P0.5 halves the size. This is the most common way to specify the scaling factor.
  • I, J, K: Specifies individual scaling factors for the X, Y, and Z axes, respectively. For example: G51 I2.0 J1.0 K0.5 would double the size in X, leave Y unchanged, and halve the size in Z.

The syntax for G50 (scaling off) is simply:

G50 ;

G50 takes no parameters. It cancels any active scaling.

4. Control System Variations: Fanuc, Haas, Mitsubishi

Let’s look at how G50 and G51 are implemented on some common CNC control systems:

  • Fanuc and Compatible Controls (e.g., Haas, Mitsubishi):

    • G51 Syntax: G51 X[center] Y[center] Z[center] P[factor] or G51 X[factor] Y[factor] Z[factor].

    • G50 Syntax: G50

    • P vs. I, J, K: Fanuc controls typically support both the P code (for uniform scaling) and the I, J, K codes (for non-uniform scaling). However, check your specific control’s manual.

    • Scaling Center: If the X, Y, and Z coordinates are omitted in the G51 command, the current position at the time of the G51 command is usually used as the scaling center. This can be very useful, but also a source of errors if not understood.

    • Modal vs. Non-Modal: G51 is typically modal – it remains active until canceled by G50.

    • Example (Fanuc/Haas/Mitsubishi):

G90 G21 ; Absolute, metric
G00 X0 Y0 Z10.0 ; Rapid to a safe position

; --- Scale up by a factor of 2, centered at X25, Y25 ---
G51 X25.0 Y25.0 P2.0 ; Activate scaling
G01 X50.0 Y50.0 F100 ;
;...Programmed move to X50 Y50, actual move to X75 Y75
G01 X0 Y0   ; 
;... Programmed move to X0 Y0, actual move to X25 Y25
G50 ; Cancel scaling

; --- Scale only the X-axis by a factor of 3 ---
G51 X0 Y0 Z0 I3.0 J1.0 K1.0 ;Different way.
G01 X10.0 Y10.0 Z5.0       ; Programmed move, X scaled by 3
G50 ; Cancel scaling
M30

5. Control System Variations: Siemens, Heidenhain, Mazatrol

  • Siemens (SINUMERIK):

    • SCALE and ASCALE: Siemens uses SCALE for programmable scaling and ASCALE for additional scaling (adding to an existing scale factor).
    • Syntax (SCALE): SCALE X[factor] Y[factor] Z[factor] (for uniform or non-uniform scaling)
    • Syntax (ASCALE): ASCALE X[factor] Y[factor] Z[factor]
    • Canceling: SCALE (without any axis parameters) cancels scaling. Do not use G50 for scaling cancel on Siemens.
    • Example:
      SCALE X2.0 Y2.0 Z1.0 ; Scale X and Y by 2, Z by 1
G01 X10.0 Y5.0 Z2.0  ; Programmed move, scaled accordingly
SCALE ; Cancel scaling
    • MIRROR: Siemens uses MIRROR for mirroring, not negative scaling factors.

  • Heidenhain:

    • SCALE: Heidenhain uses the SCALE command (or CYCL DEF 7.0 DATUM SHIFT for datum shifts, which can have a scaling effect).
    • Syntax: SCALE [factor] (for uniform scaling) or SCALE X[factor] Y[factor] Z[factor] (for non-uniform scaling).
    • Canceling: SCALE with a factor of 1.0 cancels scaling.
    • Example:
      L X+0 Y+0 Z+100 R0 FMAX  ; Rapid to safe position
TOOL CALL 1 Z S2000     ; Select tool 1
SCALE 0.5                ; Scale down by a factor of 0.5
L X+20 Y+20 Z+5 R0 F100 ; Programmed move, scaled accordingly
...
SCALE 1.0                ; Cancel scaling (set factor back to 1.0)

  • Mazatrol (Mazak):

    • Conversational Programming: Scaling is typically handled within the conversational programming interface, as part of the machining process definition. You don’t usually write G51 or G50 commands directly. You would specify a scaling factor (or choose to use the original size) when defining the machining process.
    • EIA/ISO (G-code): Mazak machines can run standard G-code programs. In this case, G51 and G50 would be used similarly to Fanuc.

6. Mirroring with Negative Scaling Factors

A powerful feature of G51 (or its equivalent on other controls) is the ability to create mirror images of a toolpath by using negative scaling factors.

  • -1.0 Scaling Factor: A scaling factor of -1.0 in a particular axis will mirror the toolpath across that axis.

  • Example (Fanuc/Haas/Mitsubishi):

    G0 X0 Y0 Z10
    G51 X0 Y0 Z0 P-1 ; Mirror in x axis.
    G01 X10
    G01 Y10
    G01 X-10
    G01 Y-10
    G50 ; Cancel mirroring.

  • Example (Siemens):

    MIRROR X0 ; Mirror across the X-axis (center of mirroring is X0)
; ... (Programmed toolpath) ...
MIRROR  ; Cancel mirroring

  • Example (Heidenhain):

     L X0 Y0 Z10
 CYCL DEF 7.0 DATUM SHIFT ; Define new datum
 CYCL DEF 7.1 X+0         ; Datum shift in X
 CYCL DEF 7.2 Y+0        ; Datum shift in Y
 CYCL DEF 11.0 SCALING   ; Activate scaling
 CYCL DEF 11.1 X-1        ; Scale factor -1 for X-axis (mirror)
; (Programmed toolpath)
 CYCL DEF 11.0 SCALING; Cancel mirroring
 CYCL DEF 11.1 X1

Important Considerations for Mirroring:

  • Tool Radius Compensation: When mirroring with G41/G42 active, you often need to switch the compensation direction (from G41 to G42, or vice versa). This is because the relationship between the tool and the workpiece is reversed.
  • Circular Interpolation (G02/G03): The direction of circular interpolation (clockwise/counterclockwise) may also need to be reversed when mirroring.
  • Control-Specific Behavior: Mirroring behavior can be complex and varies between control systems. Always consult your machine’s manual and thoroughly simulate your program before running it.

7. Best Practices for Using G50 and G51

  • Always Cancel Scaling (G50): Make it a habit to always cancel scaling with G50 (or the equivalent command for your control) when it’s no longer needed. This prevents unintended scaling of subsequent operations.
  • Use a Consistent Scaling Center: If possible, use a consistent scaling center (often the workpiece zero) for all scaling operations. This makes it easier to understand and predict the scaled toolpath.
  • Verify Scaling Factors: Double-check the scaling factors you’ve entered to ensure they are correct.
  • Simulate Your Program: Always simulate your program with scaling enabled to visually verify the toolpath and check for any errors.
  • Use Descriptive Comments: Add comments to your G-code program to clearly indicate where scaling is activated, the scaling factors used, the scaling center, and where scaling is canceled. This makes your programs easier to understand and maintain.
  • Understand Your Control: Be aware of the specific syntax and behavior of G50/G51 (or their equivalents) on your particular CNC control system.

8. Troubleshooting Common Scaling Problems

  • Incorrect Part Size:
    • Cause: Incorrect scaling factor, incorrect scaling center, forgetting to cancel scaling (G50), or scaling applied to the wrong axes.
    • Solution: Double-check the scaling factor and center point, ensure G50 is used correctly, and verify the axes being scaled.
  • Distorted Part Shape:
    • Cause: Incorrect scaling center, or non-uniform scaling applied unintentionally.
    • Solution: Verify the scaling center and ensure that you’re using uniform scaling (same factor for all axes) unless non-uniform scaling is specifically required.
  • Machine Alarms:
    • Cause: Syntax errors in the G50/G51 commands, or unsupported scaling features on your control.
    • Solution: Consult your machine’s manual for specific alarm codes, check your program for errors, and verify that your control supports the scaling features you’re trying to use.
  • Unexpected movements
    • Cause: Forgetting to cancel scaling.
    • Solution: Use G50.

9. Conclusion: Flexibility and Control with Scaling

The G50 and G51 scaling commands (and their equivalents on different CNC control systems) provide a powerful and versatile way to adjust the size of programmed toolpaths without having to modify the underlying geometry. This capability is essential for a variety of applications, from prototyping and creating part families to compensating for material shrinkage and simplifying programming. By understanding the principles of scaling, the specific implementation on your CNC control, and best practices for their use, you can significantly enhance your machining flexibility and efficiency.